Acuprep error when running sliding mesh

Junta_20361

New Altair Community Member

Dec 18, 2020

Updated Dec 28, 2020 by Junta_20361

Hello experts,

I'm trying to do the acusolve tutorial 5001 Blower Transient with HW-CFD 20.1 as the pre-processor.

I have made 2 complete model, one for the steady state (reference frame) and the other for transient (sliding mesh).

Currently, both of them can successfully run in separate.

However, when i tried to run the transient model with the initial condition taken from steady state run by using restart funtion in HW CFD.

It always interupted with AcuPrep error.

Could anyone help me solve this problem?

I have atteched 2 models for your reference.
The mesh has been removed to fits the size limitation , but the mesh controls are remained >> please regenerate the mesh.

Many thanks to you!

BlowerSteady.hm

BlowerTransient.2.Log

BlowerTransient.hm

Find more posts tagged with

English

HyperMesh CFD

Sort by:

1 - 5 of 51

acupro

Altair Employee

Dec 18, 2020

Updated Dec 18, 2020 by acupro

The RESTART functionality requires the node count remain the same from the 'initial' run to the 'restart' run. In a steady case with reference frame, the nodes on the boundary between the two volumes (MRF and Fixed) are shared - only one set of nodes. In the transient where the inner 'core' rotates, the nodes are split - one set of nodes on the boundary of the 'Fixed' volume, and another set of nodes on the boundary of the 'Rotating' volume. Thus the node count is different, and RESTART cannot be used.

Junta_20361

New Altair Community Member

Dec 20, 2020

Updated Dec 20, 2020 by Junta_20361

The RESTART functionality requires the node count remain the same from the 'initial' run to the 'restart' run. In a steady case with reference frame, the nodes on the boundary between the two volumes (MRF and Fixed) are shared - only one set of nodes. In the transient where the inner 'core' rotates, the nodes are split - one set of nodes on the boundary of the 'Fixed' volume, and another set of nodes on the boundary of the 'Rotating' volume. Thus the node count is different, and RESTART cannot be used.

hi acupro,

Verynice, now i understand why they used "project solution" command in the tutorial.

However, it seems that HW CFD doesn't have project solution command & also cannot define the initial condition base on the *.nic files like hypermesh.

Is there any solution for this?

I just want to try with HW CFD 2020.

Anyway, thank you very much for your answer!

acupro

Altair Employee

Accepted Answer

Dec 23, 2020

Updated Dec 28, 2020 by acupro

hi acupro,

Verynice, now i understand why they used "project solution" command in the tutorial.

However, it seems that HW CFD doesn't have project solution command & also cannot define the initial condition base on the *.nic files like hypermesh.

Is there any solution for this?

I just want to try with HW CFD 2020.

Anyway, thank you very much for your answer!

You are correct. There is no equivalent to 'Project Solution' yet in HyperWorks CFD. It should be included at a later date.

At present, you would need to use the 'acuProj' utility (explained in the Programs Reference Manual) and do some hand editing of the transient input file to point to the appropriate NIC files.

ipaulson

Altair Community Member

Jun 6, 2025

Has this feature been included in more recent releases of HW CFD?

acupro

Altair Employee

Jun 6, 2025

Updated Jun 6, 2025 by acupro

This 'Project Solution' is not available in HyperMesh CFD - only in SimLab.

If referring to cases specifically with rotating components (blower, fan, etc) - originally the interface surface could not also be the bounding surface of a volume assigned a reference frame. That restriction has been lifted in the last few releases. Why is that important? Now we can do an initial reference frame run using a mesh that has been split and that uses interface surface. Then we can simply restart to move to transient with rotating mesh - since the mesh has already been split and the node count will not change.

Try the following. Set up the case with the steady-state reference frame as before. But also define a rotational mesh motion for the volume around the impeller/fan, with angular velocity set to 0.0. With the outer volume fixed (no mesh mesh motion applied) and the reference volume also have the defined mesh motion - acuPrep will split the mesh and use interface surfaces. (I'm not sure if you'll need to activate mesh motion - specified, or if mesh fixed will work.) Then you should be able to define the restart run, switching to transient, and using a non-zero angular velocity. And restart should work.

Does that approach accomplish what you need?

(If you're asking for some other type of application, you may need to use SimLab with Project Solution or its equivalent - or command-line acuProj.)

ipaulson

Altair Community Member

Jun 6, 2025

Thanks for the response!

When restarting for the transient run, should the Reference Frame still be included in the model? If yes, should it have its original non-zero angular velocity assigned to it still?

acupro

Altair Employee

Jun 6, 2025

The new implementation allows for a cumulative effect - reference frame angular velocity plus mesh motion angular velocity. You could potentially make a transient run with part of the total angular velocity going to reference frame, and part going to mesh motion. This may give results closer to full transient mesh motion - but with larger time steps and shorter run time. I haven't done a lot of testing on that.

For the typical steady reference frame first - then transient moving mesh as a restart - I would recommend removing the reference frame definition - leaving only the mesh motion definition - for the transient restart run.

Sort by:

1 - 1 of 11

acupro

Altair Employee

Accepted Answer

Dec 23, 2020

Updated Dec 28, 2020 by acupro

hi acupro,

Verynice, now i understand why they used "project solution" command in the tutorial.

However, it seems that HW CFD doesn't have project solution command & also cannot define the initial condition base on the *.nic files like hypermesh.

Is there any solution for this?

I just want to try with HW CFD 2020.

Anyway, thank you very much for your answer!

You are correct. There is no equivalent to 'Project Solution' yet in HyperWorks CFD. It should be included at a later date.

At present, you would need to use the 'acuProj' utility (explained in the Programs Reference Manual) and do some hand editing of the transient input file to point to the appropriate NIC files.

View in context

Acuprep error when running sliding mesh

Find more posts tagged with

Quick Links